July 12, 2020 at 6:08 pmkmc64Subscriber
Hello, I'm getting myself confused and could really do with your help please? I have a mechanism I am simulating and trying to analyse, it's within a test bench that tests plain spherical bearings.
For the dynamic, do I need to add the motor torque as well as the rotational velocity? I don't understand what forces the software computes and what I need to add myself? When running this, I get values of force at the joints, so is this taking all connections into consideration? Such as at the top, where the mechanism is connected to the horizontal shaft that provides the oscillatory movement to the bearings, do I need to add frictional or resistant forces? Or does the system compute this? The photo shows the section I'm simulating.
Many thanks, Kayleigh
July 12, 2020 at 6:37 pmpeteroznewmanSubscriber
Hello Kayleigh, welcome to the community.
Please insert images into your posts using the Insert Image button on the toolbar because ANSYS staff are not permitted to open attachments. I did that for you here:
There is too much detail in this image to have a clear explanation of what your analysis will include and what it will exclude. As you say, it is a 4-bar mechanism, so I expect the disk at the bottom is on a motor that turns the disk.
0. Which bearings are being tested?
1. Is the motor is driven at a constant speed? If so, you don't need anything other than the rotational velocity.
The connecting rod goes up to a rocker, which has some mass.
2. Are there springs on the rocker also?
You have run this model and got out some forces at the joints. Yes, the joint force is the force needed to move the mass at the accelerations required to be consistent with the input motion.
3. Was this a Rigid Dynamics model?
Joints by default have no friction, but a Revolute Joint can include damping.
4. What is the goal of the simulation model, what outputs to you want to obtain?
The selection of joint at each location has an effect on the joint forces. For example, on the horizontal shaft, you can't use two revolute joints because that will not share the load across the two bearings on each side of the rocker.
July 13, 2020 at 9:25 amkmc64Subscriber
Okay great thank you. This is an image of the whole test bench, so yes the bottom plate is connected to the motor as shown.
0. The bench tests plain spherical bearings, there are two tested at a time shown by the red circles, there is a constant load applied to them from the back horizontally as shown. The crank rocker mechanism is to provide the oscillating frequency only.
1. Yes for each test the motor is ran at a constant speed, okay great so torque would only be required for varied speed?
2. There are no springs on the rocker no, I have just connected all sections as joints, most being rigid due to the amount of parts, then where necessary a revolute joint
3. Yes I have ran it as a rigid dynamics, it all works and moves as intended I'm just not sure that I'm applying all the correct forces or maybe I need to specify the friction at the joints were bearings are used? It's difficult because the project isn't as planned due to covid, I'm unable to get any experimental data to verify my results.
4. The whole project is slightly flawed as I'm just having to make the best of a bad situation, but the idea is that the simulation model will give me the joint forces and angular acceleration of the links when running at high speed, and then I will modify length of the links/materials etc, and hopefully come up with a modified design that will have lower joint forces/angular acceleration therefore the test bench will be more stable/less wear/less vibration at high speed.
Okay, so how would be best to simulate the horizontal shaft connecting to two bearings please?
July 13, 2020 at 6:38 pmpeteroznewmanSubscriber
What are the test specifications on the spherical bearing?
How many degrees of rotation? Is it always a constant value or does the test require exercising over a range?
What frequency of oscillation? Is it always a constant value or does the test require exercising over a range?
Those questions pretty much constrain the fixture design.
If those questions were not answered, then the test specification is incomplete and you can reduce the joint loads by simply rotating less and slower.
The Spherical Bearing could be modeled with Frictional Contact, then you would get the friction torque added to the torque required to accelerate the mass through its motion. The total torque at the motor axle can be used to select the motor size.
Please show a section view through the center of the spherical bearing in a plane that includes the cross shaft and and a horizontal spring force shaft. That way I can see which side has the ball and which side has the socket.
July 13, 2020 at 9:24 pmkmc64Subscriber
The test is to apply a constant load (340 LB) to the bearing in one direction whilst then the test bearing is rotated in one degree of freedom only. The rotation is oscillating at 20 Hz and constant, the problem the bench currently has is that it can't cope with such high speeds, so I need to modify the mechanism to help it with these high speeds. This is the whole test, it is then left oscillating at 20 Hz with a oscillation angle of +/- 6 degrees, with the load applied for 1500 hours.
Like I mentioned, unfortunately this is very different from the original plan, so I understand it's not the best, but trying to make the best of a bad situation. So really hoping I can simulate the rig with some confidence that it is representative or even a 'good' basic model of it. Then I'll still get an idea of how changing the dimensions of the mechanism affects the rig.
Okay yes, I can add in the frictional contact that sounds good. I am not entirely sure what you mean by 'The total torque at the motor axle can be used to select the motor size'. You mentioned before that I don't need to add torque due to constant speed, so is this saying take the torque from the model output to suggest an appropriate motor size?
I hope these are the images you require, the model is not mine and has several iterations on it, which is why there are some overlaps etc. When I'm simulating I remove as much as possible, but have left them in here in case they are useful to see. The test bearing is held in a rod end as shown.
Thank you so much for all this help.
July 14, 2020 at 3:27 pmpeteroznewmanSubscriber
You say the bench fixture "can't cope" with such high speeds.
Please describe in more detail what happens to the fixture as the speed is increased.
Is it that the desired speed cannot be reached, or that the noise becomes too loud, or are there other failure modes such as the connecting rod buckling?
July 14, 2020 at 3:35 pmkmc64Subscriber
Um well it's difficult because of the situation I haven't been able to see it for myself.
From what I am told, when the rig gets to 10Hz, it's vibrates 'an uncomfortable amount' and as a result of this it has never been pushed past 10Hz to the 20Hz that is required. The concern is that it will also cause damage and wear running at these speeds.
It has never been tested to the point of the rod buckling, due to safety concerns. It is capable of the speeds, it's all down to safety, with what's left of the project, the idea is to just be able to show whether the vibration and noise can be reduced or maybe damage at linkage joints can be reduced by changing the lengths of the links.
July 14, 2020 at 10:16 pmpeteroznewmanSubscriber
Take just the Rod with the fittings on each end. Use a Modal Analysis. Put a Revolute Joint to ground at each end of the Rod. What are the first six natural frequencies of the Rod?
July 15, 2020 at 10:07 am
July 15, 2020 at 10:34 ampeteroznewmanSubscriber
The first mode should not be zero, so one of the joints is not correct, but let's move on since the next mode of the con rod is 252 Hz.
You are looking for where the system has a low natural frequency that would be in the 10-20 Hz range.
One place to look is the motor sitting on the frame. You need to know the correct mass of the entire motor system that is bolted to the sheet metal form that looks like it is welded to the frame. Build a Modal analysis of the frame, sheet metal base, and motor system. You can't just use CAD, someone has to look up the mass of the motor system in a catalog, or unbolt it from the frame and weigh it.
Another place to look is the bearing loading system sitting on the top of the frame. Again, you will have to know the actual mass of the complete set of parts bolted onto the frame. Most of the parts are solid, so CAD can be a closer estimate of the true mass than the motor system, but it is best to weigh it. Build a Modal analysis of the frame and add the mass of all the parts bolted to the top. The frame structure doesn't have much in the way of a diagonal brace that prevent motion of the top of the frame from vibrating sideways, along the direction of the horizontal shaft.
Is there any instrumentation available where this fixture is located, such as accelerometers? Instrumentation can be rented, but you need someone who knows how to use it.
July 15, 2020 at 10:58 amkmc64Subscriber
Ah I see, okay that makes sense.
Unfortunately, that is not an option for me at the moment due to the circumstances. Thank you for all your help, but I will just have to take simplifications and hope that it works out using the dynamic analysis. I will just have to detail my limitations in my report.
Many thanks again for your support.
July 15, 2020 at 12:02 pmpeteroznewmanSubscriber
Please reply with your Modal analysis results of the frame with the mass on the top and we can talk about improvements.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.